advanced simulation 2

[monopolystar]

Hi all , I'm just started using NX 8.5. Recently , Im doing simulation on two ring die. i would like to simulate stress analysis of the surface contact of an inner ring insert into a outer ring.

. As you can see from the image, the upper cylinder is the inner ring while the bottom cylinder is the outer ring. meanwhile, the diameter of inner ring is slightly larger than the hole of outer ring. Anyone could help please ? i would appreciate if you comment on this mail. thanks !

 

[Tuw]

Hello Monopolystar,

Yes NX can handle press/shrink fit simulation with ease.

1. Solution used
- Sol101

2. CAD requirement
- You will need to position the CAD model, in such a away that the inner and outer ring are eccentric, the inner ring is located inside the outer ring, even though CAD interference is noticed.

3. Mesh requirement
-preferable Hex8, uniform mesh density for both rings, so that the nodes of the inner ring and the nodes of the outer ring are aligned in every angle. For example, if the inner ring diameter has 24 nodes, the outer ring diameter has 24 nodes too.

4. Surface to surface Contact definition
- between the contacting surfaces of the 2 bodies. You will need to define a "search distance" which is larger than the interference normal distance. If the interference between the CAD in radius is 1mm, you can input -2mm for example. Negative search distance means the contacting pairs will search in the opposite direction instead of its normal direction.

5. Constraint
- you can use user-defined constraint definition with reference to a cylindrical coordinate system, and fixing the theta and Z axis while freeing the R axis, or
- you can try without constraint, but 'check' on inertia relief option, that is located in the Solution Edit Settings Dialog Box

6. Loading condition
- no loading condition

And you should be able to solve.

Hope this help.
Tuw

 

[monopolystar]

hi tuw , im sincerely appreciate for your replied. It is very helpful ! Thanks a lot.

 

[monopolystar]

[/URL]]

Hi, I face some problem dealing with the setting which shown in the picture above. Which ring should I set to be source region or target region , what does that mean actually ? in addition , about the BCTSET , what do the search distance and coefficient of static friction indicate actually ? I would appreciate if anyone could comment on this post. thanks a lot.

 

[Tuw]

Hello Monopolystar,

The reason is simple. It is the default view plot setting for Solution101, that exaggerated the deformation of the simulation model for better understanding about the deformation shape. To further support my statement, you can check the overall displacement result, and the displacement magnitude should be very small...

To set the displacement scaling to actual, you will need to click the Edit Post View button, then check and set the parameter circled in picture below.

About your question on
1. Target and Source region:
In layman term, target and source region are the requirement in order for contact to occur. For example, the act of hitting the tennis ball with a tennis racket defines a contact. Whether the ball is the source or target does not distinguish much in real life. However in NXNastran, Target and Source is related with a rule as such:
"Source element's node does not penetrate the target element's surface".
With this rule, the selection of source and target becomes significantly important in terms of CAE result accuracy (Accuracy increases when penetration between source and target is minimum). Therefore, a general rule of thumb says that the source mesh should have higher mesh density compare to target mesh. If your mesh density (or element size) is same for both meshes, the selection however becomes insignificant. In your case, insignificant...

2. Coefficient of static friction:
It is the same coefficient that we learned in school. Wikipedia would do a better job explaining it than me.. Probably you can try to input a realistic value to it, and check whether the result would be different...

Kind regards,
Tuw

 

[monopolystar]

Hi Tuw , thank you for your replied. I'm confusing with the result. The inner surface of the outer ring should be having the same force with the outer surface of inner ring. But as you can see from my last post, they are not the same. I wonder what goes wrong. in addition , i would like fixed constraint of the inner ring, but i cant did it with cylinder constraint as the ring is not really a cylinder, im trying with the user defined constraint, do you mind to explain about the 6 degree of freedom ? which one should i set to be free in order to free the R-axis ? thank you. I would appreciate if you comment on this post .

 

[Tuw]

Hello Monopolystar,

You may refer to attached example .fem and .sim work files..

Kind regards,
Tuw

 

[monopolystar]

Hi Tuw,


Thanks for your replied once again. I found your file is very useful for me. thank you. In addition , I would like to input different pressure load on the surface of the hole of inner ring instead of applying same pressure load all over the surface. in other words, different nodes on the surface of the hole of inner ring will experience different pressure load. Is it possible to doing so ? Thank you. I will appreciate if could comment on this post .

 

[Tuw]

Hi Monopolystar,

For applying pressure load, it depends on the complexity of the load profile... If the loading profile has a simple pattern, probably you can save yourselves the trouble of defining a field profile with reference to cylindrical coordinate system, but instead, you can divide the surface of the inner surface into several zones, while each zone represents an average value of pressure load.. For example you can divide each 30 degree of the cylindrical inner surface, and you will get 360/30=12 pieces of surfaces, and each surface has a unique average pressure definition...

 

[monopolystar]

Hi Tuw, thanks for your kindly replied. Do you mind to have a check on my simulation ? I was trying to apply load in the inner surface of inner ring at the same time with the surface-surface contact force and the bottom corner of inner surface of inner ring should have become from compression (when only surface-to-surface contact, without pressure load) into tension. But I can't get the desired result. Do you mind to help ? Thanks. I would appreciate if you comment on this mail.

 

[monopolystar]

Hi Tuw, for your information , its a backward extrusion , thus the upper surface of inner surface of inner ring receives the lesser pressure load compared to the bottom surface. Thanks

 

[Tuw]

Hi Monopolystar,

Just had a quick glimpse on your files. I noticed that you put a contact and a glue definition into the active solution. Both definition will be effective. However, the glue definition had fixed the 2 bodies already, thus contact is not possible (could not converge as well).. Please try to remove the glue definition and see whether the result is acceptable...

Best regards,
Tuw